Category: High-Speed Machining

With additive manufacturing and 3D printers being such a hot topic these days, it’s important to remember why subtractive processes like milling are still incredibly important to rapid prototyping. But first, let’s examine some of the benefits and limitations of additive rapid prototyping (or direct digital manufacturing).

Benefits of Additive Rapid Prototyping

The process of additive rapid prototyping joins and fuses materials like liquid resins together, layer upon layer to produce a 3D object from model data. Additive rapid prototyping is generally simple, relatively inexpensive and fast. Additive rapid prototyping also allows for a substantial amount of complexity within cavities or internal areas of a part that would require undercuts and may even be impossible with subtractive processes like milling.

Limitations of Additive Rapid Prototyping

The primary drawback of additive rapid prototyping is that the resulting part usually is not made of an end-use material like metal … and even if it is, it lacks structural integrity. That’s because the point where one layer is joined to another lacks the physical strength exhibited by a solid block of the same material (with no layers or joints).

Subtractive Rapid Prototyping with End-Use Materials

Subtractive rapid prototyping provides the ability to prototype in end-use materials. Since milling or machining removes material from a larger piece of material, the finished part has a solid composition rather than a layered composition as seen in additive rapid prototyping with 3D printers. This yields a higher structural integrity which is critical if the prototype part is to be used in product testing. Product testing with a part made through subtractive prototyping allows for an accurate analysis of the part’s viability and even durability since it is made from the same material that will be used to manufacture production parts.

A Wider Range of Surface Finishes and Textures with Subtractive Prototyping

Subtractive rapid prototyping processes also offer a wider range of surface finishes for the completed prototype as opposed to the standard “stepped finish” often achieved in additive rapid prototyping with a 3D printer. This could range from a completely smooth surface with a mirror-like finish to ones with milled or engraved textures. In this way, subtractive rapid prototyping with a high speed CNC milling machine is capable of producing prototype parts with a repeatability suitable for end-use production. The smooth surface finish that can be achieved with high-speed machining can be functionally beneficial if the given part needs to slide and aesthetically beneficial if the prototype is going to be used in market testing.

Additive Rapid Prototyping vs. Subtractive Rapid Prototyping

To illustrate the points made above, we asked our applications engineers to quickly prototype a part using both additive and subtractive processes. Since our favorite after-hours (wink, wink) past time is foosball, they decided to make a “replacement” foosball man for testing. This decision was based on an actual real-life need – since we had recently broken one of the men that came with our vintage 1985 foosball table. Using additive rapid prototyping (3D printing), they were able to design a very rudimentary foosball man in about 90 minutes. From there, they began printing and in just over an hour the part seen below was complete.

Additive rapid prototype made with a 3D printer shows the typical stepped finish indicative of this process.

Using subtractive rapid prototyping (high-speed milling) programming the part took substantially longer and clocked in at 3 hrs. 45 minutes. However, milling the part below was considerably faster than 3D printing and took 28 minutes.

Well, you knew we had to “test” the part right? So, in a series of 4 rather heated games using each prototype, here’s what we found. In terms of functionality and durability, the subtractive prototype was the clear winner. Not only did it last through the 4 games, the solid composition of the part made for stronger shots with high velocity. Plus, it clearly would hold up for hundreds of more games. By comparison, the 3D printed part began to show signs of delamination on its right side half way through game 3 — and by the game 4 we had to mend it with a bit of scotch tape to get through the rest of our “product testing”. The damage to the part revealed the inside composition of the 3D printed part as seen below.

Cross section of 3D printing prototype shows internal construction.

The rather hollow nature of this part shined a bit of light on why we couldn’t achieve strong shots using this foosball man. In analyzing the resulting surface finish on both parts, we felt that the subtractive prototype was … well, simply more attractive. Plus, the milling process provided more flexibility to achieve different surface finishes. For example, we were able to make the majority of the subtractive prototype very smooth while giving the foot section a more textured finish for added “grip” or ball control. By contrast, the inherent “stepped” surface finish on the additive prototype served well in terms of ball control … but wasn’t very attractive over the entire part.

The Ultimate Subtractive Rapid Prototyping CNC Machine:

Last year’s introduction of the DATRON neo compact high-speed milling machine makes subtractive rapid prototyping more affordable and viable than ever. Plus it’s compact size and touchscreen operation make it easy to use and easy to fit in the tightest “lab-type” environment. To learn more download the brochure by filling out the form below:

So here we are. You have read all of my eloquent, informative, and groundbreaking (perhaps a minor exaggeration) blogs. You are ready. You have a pencil behind your ear and a calculator on your desk and you’re going to trust in the numbers! Slow down there cowboy, because the most important thing to remember is the numbers, formulas, and suggestions are just that – suggestions. They give you a reasonable starting point. They get you in the neighborhood but some good old CNC machinist trial and error might be in order. I know, if you bought an expensive GPS unit for your car (who buys those anymore?) and it GUARANTEED to get you within ten blocks of your destination and left the rest up to you then you might wonder why you bothered. Well my friend, if that building you were driving to was constantly moving and changing based on the simplest of variables then ten blocks isn’t too shabby. Besides, you got my Shop Math formulae for free. Stop complaining.

CNC machinist trial and error is often a necessary process even when using the most bullet-proof machining program.

Control the Variables

The point is, no matter how sophisticated your CNC machine, software, tooling, or ego is you will always have to make adjustments. Sometimes minor, sometimes major. It all depends on what you are doing and how you are doing it. There are an endless number of variables involved with machining so I won’t even attempt to touch on all of them. The name of the game is eliminating or at the very least CONTROLLING those variables to get consistent results every time. Let’s say you set up a new job on Monday morning. This job uses eight tools and takes approximately two hours. The tools do well all day Monday and when you come in Tuesday morning the second shift guy tells you he had to look busy so he swapped out all the tools. When you ask if they were worn out he replies “I dunno.” You would think they would be smart enough to put a competent human being on second shift since there is far less supervision, but trust me I know how that goes. Anyway, you have many issues now. Judging by Gomer’s attitude and general work ethic you can assume that none of the new tools were properly measured before he put them in. So it’s time to get to work – measure all your tools, check your zero points, make sure your speeds and feeds are good. Should be all set, you say? Guess again. Same program, same machine, right tools, everything looks good. That doesn’t mean it will cut the same as it did yesterday. Or even two parts ago. Depending on the tolerance you are working with something as simple as the ambient temperature and humidity can affect the final result. This is where some CNC machinist trial and error comes in.

Warming up the spindle helps to eliminate thermal expansion of the spindle as one of the variable.

Warm Up the Spindle

Before you decide a program is ready for production and release it to Gomer, you need to make some determinations. First off, make sure no matter what that you always warm up the spindle. If you warm up the spindle properly before running your first job of the day then you will ensure that thermal expansion in the spindle will not become one of your variables. That way the fifth part will come off just like the first. Also, any time your machine is going to sit more than a couple hours it is a good idea to do a warm up, especially if you are working with tight tolerances.

Know Your Tools & Standardize Your Tool Library

Another consideration when preparing a job for production is tool life, so you can avoid the problem mentioned above. By testing and running through some “CNC machinist trial and error” you will learn a lot about tool life and be able to compile some simple information and expectations. You will find that the more you do this, the faster and easier it will become. You will reach a point (especially if you followed my advice from my previous blogs and set up a standard tool library) that the information will just be there and suddenly your reference material will be right off the top of your head. Once you know your tool life you can be much more proactive in your approach to shift change and work flow.

Guideline feeds and speeds can be fine tuned through trial and error to maximize performance and cycle times.

Trial and Error with Feeds and Speeds

CNC machinist trial and error also comes into play when efficiency and productivity are the goals (when are they not?). So my suggested speeds and feeds get the part done in twenty minutes, but if I take a 10% lighter cut and increase my feed 20% then the part is off the machine faster, and my tool will last for eight parts rather than five. I have cut time, increased tool life and made the boss happy. What about QC? Are they still happy? OK, so my surface finish suffered a little, but it’s still within specifications so we are good. Success!

Trial and error with tools sometimes means pushing the envelope or even breaking a tool.

Don’t be Afraid to Push the Envelope … or Break a Tool

If there is one thing for you to remember it’s that ERROR is half of trial and error. The best machinists I ever worked with broke tools on a regular basis, just because they wanted to see what they could do. A little bit of CNC machinist trial and error, pushing the envelope, will get you farther than you may think. You will discover very quickly that the envelope is far more expansive than you imagined.

Learn More: Download the High Speed Machining White Paper:

Have you ever wondered why after milling a hole or pocket that it measures larger at the top of the cut than at the bottom? Or why your gauge pin fits nice and snug in the beginning of the hole but won’t quite make it all the way through? The simple answer is tool deflection. Everything bends. And I mean everything. Tool deflection is an omnipresent yet little understood problem. Worry not my fellow machinists, because it is not your fault! There is no eliminating tool deflection, only controlling and minimizing it. Knowledge is power, and hopefully by the end of this post you will have a working knowledge of the causes of tool deflection and potential solutions.

Simply put, tool deflection is the bending of the tool. When you cut a feature, for this example we’ll say a deep pocket. While cutting you are applying forces to the tool and the material. The material gives, which is why you get chips. However, it does not go down without a fight. When the material pushes back it forces the end of the tool in the opposite direction of the forces being applied to the material. The farther the tool sticks out, the farther the end of the tool will move.

It is possible to calculate tool deflection, but the math involved is quite complicated. If you spend any significant time in a machine shop then you know how often optimization is achieved with your eyes and ears – I consider those two things the most important tools a good machinist can have. However, if you would like to calculate some numbers for tool deflection there are multiple calculators available online. For the purposes of today’s post we will rely on our trusty eyes ears and little bit of that common sense.

Tool deflection can be reduced by using the largest diameter and lowest number of flutes possible.

Rigidity is the most important factor. As you increase the distance your tool sticks out of your tool holder the rigidity decreases exponentially. There are situations when you need the length, in which case, your best course of action is to use the largest diameter with the least number of flutes. As you decrease the diameter of your tool you also decrease the amount of force required to make it bend. Also, every flute on your cutter reduces the rigidity of your tool. If you are cutting a deep feature, you want to make sure that you are using the largest diameter the print will allow in order to optimize tool performance. Even if you need to rough with a larger diameter tool, and finish with a smaller tool in order to meet specification on your corner radii that’s OK. You also want a tool with the least number of flutes, and only stick the tool out as much as you truly need to. When researching tools, you will find that there are tools for which rigidity is a major concern and many “micro” tools come with a tapered shank to increase rigidity.

Carbide Tools vs. High Speed Steel Tools to Reduce Tool Deflection

If you think tool deflection is an issue, or you are performing cuts aggressive enough that it is causing you problems, then one thing you should always consider is carbide tooling. Aside from the benefits like higher SFPM and better tool life, carbide is about three times more rigid than high speed steel. Keep in mind however, that carbide is extremely brittle – that is not a good combination when talking about tool deflection. It takes more to deflect it, but if you provide enough force the tool is not as forgiving and will break, so beware.

As discussed in my “Climb Milling vs. Conventional Milling” blog post, cutting strategy can affect tool deflection. Utilizing dynamic toolpath strategies (see my blog post “Dynamic Milling”) can assist in minimizing tool deflection due to the light radial cut. If you rough the feature using a dynamic toolpath and make sure you are climb milling then you should be happy with your results. As discussed in these other posts, for the finish you have a couple options – either climb mill the finish or conventional mill a spring pass, or conventional mill a light finish pass with lubrication and you will be very happy with your results.

Download Cutting Tool Catalog

Hey folks, today we are going to talk about threading in multiple forms. For the most part I am going to discuss my experiences with the different types of thread cutting/forming, so if you are looking for tons of technical information I apologize, but there are so many variables when it comes to the threading –perhaps I can write a more technical blog on each type of thread forming. For now, we are going to give a general overview of cutting threads based on my experiences and opinions. I know, opinions are like… well, you get it, just stay with me and hopefully I can provide some insight.

First and foremost we have cut taps. In my experience cut taps are the most widely used across most industries. Cut taps are reasonably cheap and very versatile. You have all seen the drill charts that give you the tap drill sizes required for different threads. Pretty straight forward – drill the hole to the right size and depth, countersink the hole, then tap it. Cut taps can be used by hand, on a drill press with a tapping head, on a knee mill, or rigid tapping on a CNC machine.

Creating Threads in Through Holes with a Cut Tap

Standard tap for creating threads with a CNC milling machine.

When determining which tap you need you should pay attention to the type of hole you are tapping. When tapping a through hole you can use a standard cut tap which has a lead on it. The lead is the tapered portion on the end of the tap that essentially centers the tap in the hole when engaging.

When tapping a through hole you need to make sure you go deep enough to cut threads all the way through the hole – the length of the lead will depend on the size of the thread. The larger the thread the longer the lead.

Threading a Blind Hole with a Bottoming Tap

This bottoming tap has little or no lead and allows you to thread deeper into a blind hole.

However, if you are tapping a blind hole you would be wise to consider a bottoming tap. A bottoming tap has the lead almost completely ground off. This allows you to engage the tap deeper into a blind hole. These are used when there is a tighter tolerance on the depth of the hole, in situations where a hole too deep will break through into a feature. This is due to the main problem with cut taps … CHIPS. When using cut taps in a blind hole, regardless of standard tap or bottoming tap, you need to make room for chips. As the tap engages the hole it is cutting the thread geometry out of the material, therefore creating chips. Since you are engaging from above the chips are forced down in the hole along with the tap. If you do not provide enough room at the bottom of your hole, then you will break your tap. Simple as that. That is why bottoming taps are so helpful in blind holes – with a very short lead you do not have to drill as deep to form full threads to a certain depth. Keep in mind, there are taps available with helical geometry with the goal of lifting chips up out of the hole. In my experience, I have gotten mixed results. The complex geometry ultimately weakens the tap, so if you are tapping a tough material be careful. Just make sure you do your homework.

The Strength of a Roll Form Tap

Roll form taps like this are stronger than cut taps and forms threads rather than cutting them.

Next, we have roll form taps. When I first discovered roll form taps, I was in heaven. It was after a particularly frustrating week of broken taps and bad parts. Chances are if you are reading this then you have had some of those weeks. We all have. Roll form taps are much stronger than cut taps, and the geometry is completely different. The one drawback to roll form taps, and a major reason most shops I have worked for never adopted them completely is because the standard tap drill size no longer applies. Most standard drill charts (the large ones you put on the wall in the shop) now have standard tap, roll form tap, metric tap and STI tap drill sizes all listed separately. However, after years of using standard taps many of us don’t reference the chart as much as we should, and since the hole for a roll form tap is significantly larger than that for a cut tap, bad things can happen. A roll form tap does exactly as the name hints – it forms the threads rather than cutting them. When the tap engages the hole rather than cutting material away it changes the form of it, and shapes it into the thread geometry. If you have ever done any work for a defense contractor, this is why most prints will have a note that all threads must be formed by a cut tap. The military generally frowns upon operations that change the structure of the material, at least in my experience. They also frown upon castings as opposed to solid plates for complex parts – too much unknown in what you can’t see. Anyway, roll form taps are great. They are difficult to break (no, that’s not a challenge) but they also require a bit more torque. I have really only used roll form taps in aluminum and other soft materials, rarely in cold rolled steel. I am not sure how they perform in harder materials, but most shops don’t like the idea of two sets of drills for the same size thread, which is why they are not more widespread.

The Versatility of Making Threads with a Thread Mill

Helical boring rather than drilling combined with thread milling allows you to produce a multitude of different sized threaded holes with just two tools.

The final type of thread cutting is thread milling. Thread milling is a great operation that seems scary at first, but once you get it down it is truly amazing. There are many different types of thread mills, which I will get into in a different blog post. For now, I will discuss a single point thread mill. With a single point thread mill, you have great versatility, with most thread mills cutting a wide range of threads. You can create custom pitch threads, right hand or left hand, inside threads or outside threads all with one tool. Since I have recently started using helical boring for my holes rather than drilling, you can accomplish many different holes, with many different threads all with two tools. You bore a hole to the minor diameter of the thread, send the thread mill in to cut the threads, and you can use the thread mill itself to chamfer the top of the hole, as long as it doesn’t have to be a ninety-degree countersink, since most thread mills will be somewhere between thirty and sixty degrees. Due to the geometry of the tool, the only distance you need to make up for is from the outside edge (cutting edge, or point) of the tool to the flat tip, which is generally less than .02” on the smaller thread mills. The real benefit here is that once you mill the hole, you can send the thread mill to the bottom of the hole and mill from the bottom up, rather than top down. By doing this you are avoiding any concern of the tool running into chips at the bottom of the hole since you are moving away from the bottom of the hole. Looking at the thread mills you may not believe at first that it is going to do what it is supposed to. I know when I used one for the first time I was sure it was going to break – but it didn’t. Thread milling is the most versatile and efficient of thread forming strategies, and it is going to be my go-to from here on out unless there is a good reason I can’t do it.

Do your homework, know your tools and your materials and approach anything you do in the machine shop with a good understanding and clear head. This doesn’t change when you are threading holes. Trust the numbers, and in this case, don’t be afraid of trying new things. I always scoffed at thread milling – I only wish I had found it sooner. Stay safe folks.

Download Cutting Tool Catalog

If you have spent any considerable time in a machine shop I am sure you have heard the term “dynamic milling.” There are many other names out there depending on the CAM software you use – Edgecam calls it “Waveform” while Surfcam calls it “TrueMill.” Solidcam calls it “iMachining” while Mastercam calls it “Dynamic Milling.” You get the point. Every CAM package will claim theirs is the best, and while they may approach certain cuts differently, they are all based on a simple principle that in practice will give you amazing results. I have been a machinist and CNC programmer for ten years, and my first experience with dynamic toolpaths had me speechless. Today I hope to open that same door for you.

Each CAM package calls their dynamic milling function by a different name … and most of them will give you very favorable results.

Dynamic toolpaths are not a new concept by any means. There is a very good reason many machinists have long used light depth (axial) cuts with heavy side (radial) cuts to achieve their machining goals. Any machinist who has been in the industry more than 25 years remembers a day when CNC was the minority. Current CAM software allows for significantly more complex and lengthy programs and precision. When you are turning handles on a Bridgeport maintaining a 10% step or a specific chip load would be impossible with dynamic motion involved. Can you imagine hand writing and punching tape for a 600,000-line G-code program? It’s been done, but it certainly can’t be called efficient. So it’s not for a lack of knowledge, simply a lack of technology that dynamic toolpaths are not standard practice … yet.

Maximize Tool and Spindle Life with Dynamic Toolpaths

Dynamic strategies have a very simple principle – maintain a constant chip load throughout the entire cut utilizing a full depth (axial) cut and very light side (radial) cut. The benefits you will see from this type of cut include longer tool life, longer spindle life, improved surface finish, greater efficiency and awesome rooster tails. No really though, I’m not joking. You are going to have people standing there watching the machine run just because of how the chips are flying.

Dynamic toolpaths help to extend the life of your machining spindle as well as your cutting tools.

First and foremost is tool life. I will also throw spindle life in with tool life because they really go hand in hand. You get multiple benefits for both your tool and spindle if you properly apply dynamic strategies. If you are cutting a pocket or any internal feature that doesn’t allow an approach from outside the material, then entry into the cut is not only the first consideration, but one of the more important. I always use a helical entry motion with a 1%-3% helix angle, or entry angle. You want to use an entry diameter that is somewhere between 120% and 150% of your tool diameter – be careful, sometimes the CAM software asks for a radius rather than a diameter and that information makes a huge difference. Once you are at depth the real fun begins. Due to the light radial cut you can really be aggressive with your feed rate. Depending on the limits of the spindle RPM, use the tooling manufacturers specifications on chip load and surface feet per minute (check my blog on shop math). In my first experience with a dynamic toolpath I was running a 3-flute .500” end mill with a 1.5” flute length. The cut was 1.375” deep, with a 10% (.05”) step over with a feed rate of 144 inches per minute. I used a high helix end mill to assist in chip evacuation which created a “rooster tail” of chips trailing the cut. It was a thing of beauty. Even though the cut was so fast and seemingly aggressively deep, the tool lasted through 32 parts and gave the same finish on part 32 that it had given on part 1. The full depth cut means that you are wearing the entire flute length evenly, therefore you are not going to get lines on your finish. The light radial cut reduces the cutting forces, thereby reducing overall wear on both the tool and the spindle.

Efficiency is also a significant benefit. Pretend for a moment that you are cutting a 1.375” deep pocket with features at 4 different depths. Using a standard toolpath and a light depth with a heavy step over you will cut from the top of your part down. Depending on how aggressive you are with your step down you will cut many passes on each depth, with the deepest being the most time consuming. Utilizing a dynamic strategy you will cut from the bottom up, meaning each depth will consist of one pass, with all previous passes having already cleared out other material at that depth. Therefore, at each depth you are only cutting the remaining material, essentially creating a “rest rough” toolpath that minimizes total machining time.

With dynamic toolpath strategies you will not only improve tool life, spindle life and surface finish but also overall cycle time and cost efficiency. Not to mention you will impress the boss and anybody else who happens to walk by. Do me a favor, and give it a shot. You won’t be sorry you did.

Download Cutting Tool Catalog

This may seem like a strange topic for a blog post. Burrs, really? Snorefest, am I right? I understand, trust me. Let me ask you one question before you move on to the next post, what do you do to your parts after they come off the machine? Depending on your coolant you wash them, then are they ready to go to inspection? No sir, nine times out of ten they are not. When the part comes off the machine there is almost always some form of deburring operation. Unless of course the programmer includes small chamfers on your part as a deburring operation inside the program. Either way, when you spend as much time as you do performing a single omnipresent function, how could it be as trivial as everyone seems to think? I have worked from prints dating as far back as 1938, and even that print had a note on it requiring all sharp edges and burrs be removed. This post is intended to shed some light on the often ignored topic of burrs, and perhaps teach you a bit in search of strategies aimed at eliminating, or at the very least minimizing burring on your machined parts.

Burrs are a concern for multiple reasons. First and foremost, they can cause dimensional issues or fit issues. The dimension on your part may be right on, but if there is a burr on the edge then subsequent parts may not fit. Along those same lines, depending on the location of your burr you could have a part that is in fact within tolerance, but measures out of spec because of burring. Another major concern when dealing with burrs is cost. Deburring, like inspection, is not a productive operation – you are not producing parts, simply making the parts that you already produced meet requirements. Since the operation itself is not making money, it must be costing money. You know how it works – if it costs money, do less of it. It doesn’t matter how unreasonable the request may be, just do the same thing you’ve always done. Only, do it faster. And for less money. And with no overtime. I digress – deburring operations can be reduced, which will make you more efficient and your department more profitable. Many studies have been done on the causes of burring, and one of the reports I read was somewhat eye opening. On a part of medium complexity it is estimated that deburring accounts for 14% of the total manufacturing cost.

Sharp tools reduce burrs and for that reason it is a good idea to use a different tool for finishing than the one used for roughing.

There is a lot of money to be made by optimizing strategies and tooling selection. One of the more common culprits is the tool you are using. Always make sure your tools are sharp, since a dull tool can cause serious burrs even with the optimal tool path. In fact, watching for burrs is one of the best ways to monitor tool life, at least until you have a good understanding of how your go-to tools are going to perform. Also, this is one reason it’s a good idea to use a different tool for finishing than you do for roughing – that way you ensure the best finish and also limit burring.

Minimize Burrs in CNC Drilling Applications

Burrs when drilling can occur because you haven’t drilled deep enough to account for the angled tip.

When it comes to drilling, many of the same rules apply. A dull drill is going to give you larger burrs on the bottom of your part when you drill through – fresh drills will help with that. One of the simpler causes of burrs when drilling is not drilling deep enough. When you are drilling through your part you need to make sure you make up for the angled tip – the larger your drill diameter the deeper you will need to go. Drilling too shallow will result in what almost looks like a cap on the bottom of your part, not to mention a taper at the bottom of your hole. If you drill deep enough with a good, sharp drill you should be good to go.

Burr free drilling can be achieved by maintaining sharp tools and accounting for the angled drill tip when drilling through holes.

Burrs are a frustrating, time consuming problem that you will always deal with on some level. Just take care of your tools, mind your feeds and speeds and make sure you are drilling deep enough. It can be more efficient to utilize your CNC machine to deburr in process, just keep in mind there will always be geometry that you will need to deburr by hand. Get next to it folks, cause it’s never going away. Just keep it under control. Until next time, be safe and mind the numbers.

Download Cutting Tool Catalog

Push Your Program to the Limit with Balanced CNC Tools.

I talk a lot about optimizing programs, some would say too much. I go on about it to lull my children to sleep. Though, I think there are worse subjects to obsess over. So, with that aside, let’s talk a little about tooling – specifically balanced CNC tools.

If you use a DATRON or any other HSC machine, you may be familiar with our line of single flute end mills. Most traditional machinists would utilize a single flute end mill for cutting soft materials, like thermoplastics or acrylics, but the geniuses at DATRON AG developed a line of single flutes specifically for milling non-ferrous materials, specifically aluminum. Coupled with a high RPM and a fast feed rate, our single flute cutters have a reputation for devouring aluminum at an impressive pace.

With high RPM being the most important feature to accompany a single flute end mill, DATRON had something clever in mind to combat vibration with larger diameter end mills (>6mm). DATRON calls it “Specially Balanced”.

Balanced CNC tools like this specially balanced single flute end mill help to mitigate vibration.

As you can see in the picture, a healthy amount of material is removed from the backside of the cutting edge to balance the tool. What does this mean for the end user? A couple of key points:

Reduced vibrations = reduced chatter marks

Balanced tool = Higher RPM and higher feed rates

Standard toric cut + Balancing = Long reach milling

For optimizing purposes, this is tremendous, since you can run the same diameter at 50% higher RPM, and therefore a 50% increase in feed rate while maintaining the same chip load. So, if you have a roughing operation in your current program that uses a 6mm single flute end mill, at 32,000 RPM and 2 meters a minute, replace the end mill with a balanced unit of the same size, and you can bump up your RPM and feed rate by 50%.

Just as well, if you have a situation where you need to mill a deep pocket, these tools can be a life-saver. Take this vacuum adapter we made:

This vacuum adapter was made using a specially balanced single flute end mil for deep pocket milling.

At 1.75” deep, a 10mm balanced single flute had no problem removing all material from the inside of the cavity as well as cutting the part out on a vacuum table and left no chatter marks. DATRON offers balanced end mills that go over 3” deep, so you’re not too limited on what you can accomplish.

So, on your next project, consider a balanced end mill for your all your roughing, finishing, or deep milling needs.

Download Cutting Tool Catalog

If you visit ten machine shops you will more than likely find ten drastically different approaches to setup sheets and documentation procedures. Every one of them is the best. Just ask. Proper and organized documentation and setup sheets are vital to the efficient operation of any shop, and adding multiple shifts and operators or programmers running multiple machines multiplies the necessity exponentially. As with literally almost everything you do in the machine shop, there is no black and white. I’m not going to tell you which way is the best, because there are too many variables. I am simply going to make some suggestions based on my experiences. I’m not going to lie, as I’m sure you have experienced firsthand, change is never easy. Especially when you are dealing with the old salt that’s been doing this for 50 years. You know the guy – same denim apron every day, same bologna and cheese sandwich for lunch (always at 11:45 instead of 12, just to be difficult), coffee at 9 and bathroom at 9:30. You get the point. It’s going to be an uphill battle, but it will be worth it. If not, just wait until he retires. It has to happen someday.

If possible, standardize tools keeping them in the same position from one machine to the next and leaving two open “variable” spots in the tool changer.

My first suggestion is standardizing tools. This is mainly a concern in CNC shops since you are manually loading tools on your manual machines anyway. The first step in standardizing your tools is accomplished in your CAM software. The tool database needs to be created. I would always suggest starting from scratch. As you program jobs and figure out which tools are the most common the picture will become clear. Make a tool database that only holds the tools you use – it makes programming much simpler rather than having to play with filters and tool types. It may take time to decide what works best for your shop but if Tool 1 is a 6mm single flute end mill on machine 1 it should be the same on all of your milling machines. The last machine shop I worked in ran tools in numerical order for each job. I would run anywhere from two to six jobs a day, and each job used a different set of tools. Every job started at Tool 1, and unless it was a lucky day that tool was different from the last Tool 1. Some of these jobs used upwards of twelve tools. On a busy day (six jobs, twelve tools each) you are loading seventy-two tools by hand. That doesn’t include any tools that needed to be changed in the holder. Very inefficient. Now let’s say we standardized our tools. In every machine in our shop Tools 1-10 are the same, and we will leave two positions open for variables. Tool 1 here is the same as Tool 1 over there. Got it? OK, now on that same busy day with six jobs, each using twelve tools you are loading up to twelve variable tools by hand. Twelve is more efficient than seventy-two (you can refer to my blog on shop math if necessary, but I think you see my point). You will have so much time to research sleepers in your fantasy football league that you are a shoe-in for the championship. You’re welcome.

Setup sheets can be as simple as a file folder or manila envelope detailing everything in pencil so that you can make revisions as you go.

The next topic to discuss is the actual setup sheet. This is a sheet that should accompany the job on some level. To be honest my preferred method for this has always been a filing cabinet with manila folders. I know, digital age and all that. There is a place for that, but especially when you are trying to assimilate old guys who still aren’t quite sure how to check their email sometimes relying on digital paperwork can be difficult. If the other programmer saves a file in the wrong location or makes changes without telling you then the whole system can fall apart. Program a job, take a PENCIL (no pens!) and document the details. My setup sheets always included the part number, fixture location, tooling list, and a brief description of the setup including the X, Y and Z zero points and any pertinent information on fixture location or operation. Using a pencil was always an important aspect for me because not only can you modify what you write but you will be able to see if somebody else made a change and “forgot” to tell you. The old guys get nostalgic with pencils too. It puts them at ease, makes them a little more docile and cooperative. I’ve experienced mixed results with that last point, so be wary. Anyway, the point here is that you get a work order and you can go to your filing cabinet to pull that job number. You can write the current revision level on the folder itself or the setup sheet to keep compliance happy, and when the job is done it goes back into the filing cabinet. You can most definitely make an argument for doing this all digitally, and if you have a good system it is probably the way to go. With a digital system you don’t have as much paper floating around, you don’t have to worry about physical damage (losing documentation in a fire for example) as long as you back everything up, preferably on an off-site server. Digital documentation management is also more efficient since you are pulling the document off the same server you are pulling your program, all at the same time. I have yet to use a digital system that didn’t have problems, hence my preference for the old filing cabinet but if you can manage a digital system and avoid any major headaches you are ahead of the game.

Notate everything in your job setup sheets and documentation so that other machinists who may step into a job know exactly what has been done.

Finally, I will talk about documentation. This one is easy. You will be using the folder and setup sheet that we already talked about, which has all of the information on it that we already talked about. The point here is document everything. While you were running the job on third shift Tool 2 was chattering a lot so you changed out the tool and slowed your feed rate. They lost power briefly on first shift so they had to reload the program. How will they know what changes they need to make? I’ll tell you! When the first shift operator came in this morning you were drooling on yourself so much he couldn’t understand any of the words coming out of your mouth, but he’s too nice to say anything. Instead, he checked the setup sheet and saw the detailed note you left about the issue you had and how you fixed it. Good work! Now just in case you never updated the server he can make the change permanent and we’re done. See? I was able to teach you something after all. DOCUMENT EVERYTHING, no matter how small or insignificant it may seem. As I have stated before, it’s usually the small stuff that makes the difference. There is always a different way to do things and the people who can recognize where their process is lacking are already ahead of the game.

Download Cutting Tool Catalog

So, if you’ve been reading this blog, or cruising through our website, then I’m fairly sure you’re aware that we make an extremely capable CNC vacuum table. It’s the must have fixture for many industries – rapid prototyping, signage, front panels, etc. Where the vacuum table can truly shine is holding very small parts.

I once ran a demonstration for a prospective customer that showed that you can cut an entire 12” x 18” sheet of 0.020” thick aluminum into 6mm discs without having any of them fly off the vacuum table. See video below as an example. You can see that the last cut on the perimeter of these small parts goes through the sheet material exposing our VacuCard paper that sits between the sheet stock and the vacuum table – serving as a sacrificial layer that allows you to cut through the workpiece but not into the top of your vacuum table.

With all of this being said, vacuum tables are an excellent workholding solution, but they require a certain approach to get the most out of them.

1) Vacuum Table with Regular or Dense Hole Pattern?

Vacuum Table Tops can be ordered in the standard hole size (right) or in the dense hole pattern (left) which is designed to hold particularly small parts without having them fling off the table when they’re milled free of the sheet material.

The first defining feature of our vacuum tables is the density of the vacuum holes. We have two patterns, regular and dense. The regular pattern is well suited to most of our applications, but when you get down to parts smaller than a square inch, or a more difficult to cut material, a dense hole table is a good choice. The key to the dense hole plate is having more than twice as many holes as a standard plate, thus allowing better suction on smaller parts.

2) Use Vacuum Table Paper

Vacuum table paper known as VacuCard is air permeable but thick enough to allow you to mill through the workpiece without milling into the surface of the vacuum table.

The next step may seem like a no-brainer, but it’s especially important for very small parts. Once a piece of our vacuum table paper (known as VacuCard or VacuFlow) has been cut into, it becomes ineffective for smaller parts. Cuts in the paper allow a path for air to leak by, as well as leave a raised edge that prevents the material from sitting flat on the table.

3) Vacuum Table Strategy

Vacuum table strategy includes both onion skinning and tabbing methods to limit cutting force so that the workpiece stays on the vacuum table.

One of the single most important methods of holding small pieces on the vacuum table is your strategy. If you are a little too gung-ho and try to take out a small piece in one pass, you’ll likely have cutting forces too high for the vacuum to overcome. I always recommend two methods; Onion Skinning or Tabbing. Either one works quite well, simply leave a small amount of material at the bottom of your piece to take out at the end of the operation. This will greatly reduce cutting forces and prevent unnecessary scrapping of parts.

4) Tools for Use with a Vacuum Table

Vacuum Table tool selection obviously is made based on the required process or cut, but in general, the smaller the better … and consider downcut tools for finish cuts.

Use a carefully picked tool in conjunction with step 3 to increase your likelihood of success. My weapon of choice is typically an end mill that is a third the diameter of my original tool, combined with a high RPM and moderate feed rate. With such a small tool, your cutting forces reduce even further to prevent movement of the material. For very stubborn pieces, consider using a down-cutting end mill for finish cuts. Downcut tools push the material down while milling, instead of pulling up, which helps small pieces stay-put.

5) Mill Recessed Areas in Vacuum Table Sacrificial Layer

Vacuum table sacrificial layer that can be milled with recessed areas so that your part is held in place by vacuum suction as well as physical support on the sides of the workpiece.

So, your part just isn’t holding, you’ve done everything you could, but it’s not happening. Don’t worry. There’s hope. First, to get the part to a state where it will hold on the vacuum table – you may need to leave some material, but that’s OK. Next, get yourself some MagicBoard, or a porous aluminum. Both have excellent machinability, rigidity, and the ability to let vacuum flow through them. Take either of these materials and mill a cavity into it to retain your part. Now you have physical support on the sides to prevent part movement, which allows you to cut very small parts, very quickly.

So, that’s pretty much it. With a lot of practice and a little patience, using these basic guidelines will find you well on the path to machining some very intricate parts on a very small scale. To learn more about DATRON vacuum tables and other workholding accessories feel free to download this brochure.

Download CNC Workholding Brochure:

Absolute vs. Incremental Movement? These are two terms that you will hear or use in the machine shop, and there are many people who don’t really understand the difference. When I am in a customer’s shop training them on their new machine, it’s a little surprising to me how many people don’t know what the distinction is. Don’t get me wrong, there is nothing wrong with not knowing – after all, if you already knew then you wouldn’t be reading this right now and then my existence would be meaningless.

Absolute vs. Incremental Movement

In my experience there are a couple ways to convey the difference between absolute movement and incremental movement. When it comes to machine movement, simply put:

An ABSOLUTE movement moves TO A COORDINATE based on your ZERO POINT.

An INCREMENTAL movement moves A DISTANCE based on your CURRENT POSITION. An incremental movement does not take your part zero point into consideration.

Absolute Movement – used to move the machine from a random location at the back of the work area to the zero point (in this case, top of the left front corner on the workpiece).

Let’s run through an example. We will work on the assumption that you have a fixture and work piece set up on your machine, and your zero point is the front left corner, with top of stock being Z zero. You just finished setting up your tools so you are located near the back of your table at some random coordinate. We will pretend that your program starts from X0 Y0 Z0.5. So here is your dilemma – you are currently at X6.753 Y14.265 Z2.37 and you need to get to X0 Y0 Z0.5. How will you do it?

Absolute vs. Incremental?

Well, technically you can use either absolute movement or incremental movement. To make this incremental movement you would enter X -6.753 Y-14.265 and then you do some math. You are currently at Z 2.37 and need to reach Z 0.5. 2.37 – 0.5 = 1.87. So for your Z input you would enter Z -1.87. This would get you to X0 Y0 Z0.5. On the flip side, if you make an absolute movement your input will be X0 Y0 Z0.5. You are telling the machine “I want to move the X axis to 0, I want to move the Y axis to 0, and I want to move the Z axis to 0.5.” This is where the real benefit of an absolute movement comes in. When you are moving TO A POINT absolute is the much simpler way to go.

Incremental Movement – used after milling a hole in a part and needing to mill another feature 6″ away.

On the other side of this argument, is the situation where you have drilled a hole or pocket in your part, and you know that you need another feature six inches away. Now, if your first feature is at X0 Y0 then it’s really not a concern, since both absolute movement and incremental movement would be the same. However, if you are not at zero, then suddenly your absolute movement becomes more difficult as you need to determine a point in relation to your zero point, rather than a distance from your current position. Let’s use the same numbers as before. You drilled a hole at X6.753 Y14.265. You need a second hole six inches away in the X axis. In order to use an absolute movement your XY input would be X12.735 (6.753 + 6.000) Y14.265. Not too complicated, but certainly there’s a possibility for error. On the other hand, if you choose to do an incremental movement your XY input is X6 Y0. You are telling the machine “I want to move the X axis 6 inches in the positive direction, and I want to move the Y 0 inches.” With incremental movement you are telling the machine A DISTANCE.

It is altogether possible that I just made this more confusing for you. This is not an easy thing to understand at first, and as I have found in my training of others, it is not always an easy thing to teach. Hopefully what I said makes sense – if not feel free to comment and ask any questions you may have. Understanding the difference between absolute and incremental can make your job a whole lot easier and more efficient.